Pro/ENGINEER FAQ 2009

Too much info, I know — this post is the result of some keyword investigation I did with “pro/e”. Turns out “pro/e spiral” is a popular key word, so I figured “I can do that; it might be fun.” It’s also a throwback to the old PTC certification program where something like this was required. And, it gives me a chance to add a link listing advanced trig functions you can use in relations: necessary if you have an interest in the “golden spiral”.

Doesn't end on a rectangular boundary, but that's the equation

Pro/E Relations:
b = .0053468
r = exp( b * theta )
theta = 360 * t
z = 0

I always believed Pro/E retrieved files in this (classic) order:

1. In session (in memory)
2. Current working directory
3. Directory containing the assembly or drawing file
4. Directories in the search path

According to this TAN, Wildfire changed the search order to:

1. Pro/ENGINEER session
2. the Search/Retrieve directory where the parent object was found
3. Active Intralink/Windchill Workspace and Commonspace
4. Local Working Directory
5. Search paths …

Note reversal of working directory and parent object directory.

Thanks to the PTC/User Exploder.

Which of these rounds do you prefer?

I prefer the round on the bottom. Similar to surface modeling practices, 4-sided patches are preferred to triangular patches.

The quad patch transition on the bottom is a result of sweeping a smaller radius around a larger radius. A difference of only 10% in radii is enough to create a desirable transition.

The triangular patch transition on the top is a result of the opposite condition: an equal or larger radius is swept around an equal or smaller radius. Most users consider this transition to be the normal case, but the reality is that the triangular patch can create self-intersecting geometry (a.k.a. geometry check) that is not obvious but can cause problems later.

If you can’t force yourself to vary radii values to create the swept round transition on the right, at least be careful to avoid geometry checks with constant round values. After all, who’s actually going to care if a round is .01″, .011″, or .009″?

There was a pretty good discussion of absolute vs relative accuracy on the exploder recently, so I thought I’d chip in with my 2¢.

1. I think absolute accuracy is better understood than relative accuracy.
2. I think accuracy and regen times have lost significance for a lot of Pro/E users as hardware has improved.

Some old posts on accuracy

Now, as far as creating useable models and drawings derived from those models:

If you have a standard title block tolerance or a standard set of tolerances according to part types or manufacturing processes that limit the precision of your drawings, I think you’re actually hurting yourself if you design (model) outside the limits of your drawings. I sometimes run into problems with rounding errors caused by created dimensions, but modeling to 10X the accuracy of the created dimension avoids this problem. Easily said, not easily accomplished by a lot of users.

My suggestion is that if your title block limits you to .01mm precision, then set your absolute accuracy to .001mm. Set your default sketcher decimal places to 2, and your default decimal places to 3. Avoid the temptation to specify dimensions with greater precision than necessary.

Precision costs money at every step of the design process. Engineers are loathe to leave small gaps or misalignments, but that’s the reality of manufacturing. Start thinking in terms of real world fits and tolerances, and suddenly those gaps and misalignments won’t look so bad. If they do, change the design to accommodate them.

Absolute accuracy would be fairly easy to implement in start parts, which could be assigned different values according to end use; sheetmetal might not be as fine as plastics, etc.

Remember that some users will have trouble with geom checks as accuracy requirements increase, so keep an eye out for geom checks, especially in surface models. Vigilance and training are the answers.

Here’s a link to an old topic that came up at work this week. I finally got a chance to solve the problem using Behavior Modeler and it seems pretty slick, but simple relations work just as well, and make for a simpler model.

 I have had problems in the past with the new mass property parameters, but hopefully these have been resolve. Just to be safe, I would double-check these relations against the info in the Model Analysis (old, but reliable). I wouldn’t assume that these relations are “set and forget”!

Update: Here’s another instance of the PTC/User forums showing me that I’m out-of-date:

If you want an ordinary offset coordinate system, highlight the “destination” coordinate system first and then create a new coordinate system in your target part. Pro/E will create offset dimensions to the next coordinate system (“source”) you pick, eliminating the need to measure a transform.

NOTE: The resulting feature is modifiable; it’s not the same as a coordinate system created from file. Modifying transforms can be difficult; I might prefer the “from file” technique in some situations.

The first time I came across a coordinate system created from a transform, I was stumped. I couldn’t figure out how to modify it, so I decided it was too obscure a technique for general use. I eventually got over myself, and since then I’ve discovered quite a few uses for a solid anchor datum for subassemblies and components. The beauty of a coordinate system created from a transform file is that there are no dimensions to accidentally modify.

I never did get used to the “fix” constraint, so I sometimes package an organic part and then create a transformed coordinate for assembly. I also use transforms to create coordinate systems for customers to simplify import into foreign cad systems.

Transforms are also great for providing stable references for major subassemblies, such as engines or cabs, and mounting optional components such as alternators, water pumps, etc.

You can always move a component, re-measure the transform, and redefine the transformed coordinate system later. It’s not that complicated, once you’ve done a few.

Analysis > measure > transform [part csys, assy csys].

Open the info window and do a “File > Save As” to save the transform for later.

Insert > Model Datum > Coordinate System. Choose “From File” for the “Offset type” and load the saved transform file.

My mantra used to be “You’re only as good as your last save”, and that probably works well for most people.

Recently, though, I’ve decided that “3-2-1″ is more important and fundamental for most people. Pro/E users deal with the 6 Degrees of Freedom in multiple ways: assembly, sketching, geometric tolerancing, and advanced features. For example:

Geometric tolerancing: Primary, Secondary, Tertiary datums can be defined by a plane, a line, and a point. Even though people commonly specify three planes, individual contributions are limited by the order of specification.

Assembly constraints: Mate and insert can be defined by a flat surface (plane) and a cylindrical surface (axis). Orientation can be added with a surface, but aligning points will fully constrain the assembly as well.

Sketching: Obviously, the sketch plane provides the first 3 DOF (1 translation and 2 rotations), but have you ever used a normal edge to define the sketch orientation? In reality, the sketch orientation reference is 1 DOF (orientation), and the sketch provides the last 2 DOF (2 translations).

Variable Section Sweep: “Section plane control” provides two rotation constraints normal to the curve and the location along the curve adds a translation constraint. “Horizontal/vertical control” is the orientation constraint. The sketch provides the last two translation constraints, as in an ordinary extrude.

Understanding the 6 Degrees of Freedom will make Pro/E work more understandable, efficient, and robust. Think about the constraints you choose during your next assembly -try to select a surface (3) first, then add another vector (2) such as an insert or align to an edge or axis, and finally an orientation (1). Same thing with your geometric tolerances.

If you get into trouble with advanced features like variable section sweeps, be sure to deconstruct the 6 Degrees of Freedoms.